HSMWorks 2017 / Solidworks Prem 2017 - 2D Chamfer problems

[Anonymous]

I am having issues creating simple chamfers.  I've used both the chamfer tool path, and also the contour tool path, both with the same results.

No matter what I do, my chamfers are all at least .05" - huge!  

I am commanding a .01" chamfer.

Tool is touched off on a Renishaw OTS.

Why are the chamfers coming out so **** huuuuge?

The cutter is a 4fl carbide 90 deg chamfer mill

[Laurens-3DTechDraw]

---

@lenny_1962 wrote:

PUT UP THE FILE!!

---

And give us the name/number of the tool.

Both would be great.

[Anonymous]

Attached.  Its an assembly

[lenny_1962]

looks fine, what does the gcode look like?

what machine are you posting too?

here is mine to a haas, g54 and had to change tool number

%
O33
(CREATED: TUESDAY, MAY 23, 2017 11:36:08)
(T20 D=0.375 CR=0. TAPER=45DEG - ZMIN=-0.075 - CHAMFER MILL)
G17 G40 G80 G90
(T20 CHAMFER MILL)
T20 M6
S5000 M3
G54 G0 X3.1885 Y-0.9814
G43 H20
Z0.6
M8
Z0.14
G1 Z-0.0206 F13.333
Z-0.0375
Y-0.9812 Z-0.042
Y-0.9804 Z-0.0465
Y-0.979 Z-0.0508
X3.1884 Y-0.9772 Z-0.0549
Y-0.9748 Z-0.0588
X3.1883 Y-0.972 Z-0.0624
X3.1882 Y-0.9688 Z-0.0656
X3.1881 Y-0.9653 Z-0.0684
X3.188 Y-0.9614 Z-0.0707
X3.1879 Y-0.9573 Z-0.0726
X3.1878 Y-0.9529 Z-0.0739
X3.1877 Y-0.9485 Z-0.0747
X3.1876 Y-0.944 Z-0.075
X3.1866 Y-0.9065 F40.
G17 G3 X3.1481 Y-0.87 I-0.0375 J-0.001
G1 X3.1373 Y-0.8702
X3.1295 Y-0.8708
X3.1217 Y-0.8719
X3.1139 Y-0.8733
X3.1064 Y-0.8751
X3.0963 Y-0.8782
X3.0869 Y-0.8818
X3.0777 Y-0.886
X3.0672 Y-0.8918
G3 X2.995 Y-1.02 I0.0778 J-0.1282
G1 Y-1.125
G2 X2.375 Y-1.745 I-0.62 J0.
G1 X1.625
G2 X1.005 Y-1.125 I0. J0.62
G1 Y-1.02
G3 X0.9325 Y-0.8916 I-0.15 J0.
G1 X0.9241 Y-0.8869
X0.9168 Y-0.8834
X0.9092 Y-0.8802
X0.9015 Y-0.8774
X0.8943 Y-0.8753
X0.8841 Y-0.8729
X0.8744 Y-0.8713
X0.8646 Y-0.8704
X0.8511 Y-0.8699
G3 X0.8124 Y-0.9062 I-0.0012 J-0.0375
G1 X0.8112 Y-0.9437
X0.8111 Y-0.9482 Z-0.0747
X0.8109 Y-0.9527 Z-0.0739
X0.8108 Y-0.957 Z-0.0726
X0.8107 Y-0.9611 Z-0.0707
X0.8105 Y-0.965 Z-0.0684
X0.8104 Y-0.9685 Z-0.0656
X0.8103 Y-0.9717 Z-0.0624
X0.8102 Y-0.9745 Z-0.0588
X0.8101 Y-0.9769 Z-0.0549
Y-0.9787 Z-0.0508
X0.81 Y-0.9801 Z-0.0465
Y-0.9809 Z-0.042
Y-0.9812 Z-0.0375
G0 Z0.6
M9
M5
G0 G91 G28 Z0.
G28 Y0.
G0 G49 G90
M30
%

[Anonymous]

Mine is an Okuma Genos M560V, P300 control.  Using generic Okuma post.

%
O2651
(GP600 Upper Pipe Clamp OP1)
(T996 D=0.375 CR=0. TAPER=45deg - ZMIN=-0.06 - chamfer mill)
N1 G40 G80 G90 G94 G17
N2 G20
N3 G30 P02

(2D Contour9)
N5 M09
N6 G116 T996
N7 S5000 M03
N8 G15 H30
N9 M08
N11 G00 X3.1861 Y-0.9819
N12 G56 Z0.6 H996
N13 Z0.14
N14 G01 Z-0.0206 F13.333
N15 Z-0.0225
N16 Y-0.9816 Z-0.027
N17 Y-0.9808 Z-0.0315
N18 Y-0.9795 Z-0.0358
N19 X3.186 Y-0.9776 Z-0.0399
N20 Y-0.9753 Z-0.0438
N21 Y-0.9725 Z-0.0474
N22 X3.1859 Y-0.9693 Z-0.0506
N23 X3.1858 Y-0.9657 Z-0.0534
N24 Y-0.9618 Z-0.0557
N25 X3.1857 Y-0.9577 Z-0.0576
N26 Y-0.9534 Z-0.0589
N27 X3.1856 Y-0.9489 Z-0.0597
N28 X3.1855 Y-0.9444 Z-0.06
N29 X3.1849 Y-0.9069 F40
N30 G03 X3.1469 Y-0.87 I-0.0375 J-0.0006
N31 G01 X3.1403 Y-0.8701
N32 X3.1357 Y-0.8703
N33 X3.131 Y-0.8707
N34 X3.1264 Y-0.8712
N35 X3.1218 Y-0.8718
N36 X3.1171 Y-0.8726
N37 X3.1125 Y-0.8736
N38 X3.1079 Y-0.8747
N39 X3.1028 Y-0.8761
N40 X3.0975 Y-0.8777
N41 X3.0929 Y-0.8793
N42 X3.0884 Y-0.8811
N43 X3.0839 Y-0.883
N44 X3.0795 Y-0.8851
N45 X3.0751 Y-0.8873
N46 X3.0708 Y-0.8896
N47 X3.0661 Y-0.8924
N48 X3.064 Y-0.8937
N49 G03 X2.995 Y-1.02 I0.081 J-0.1263
N50 G01 Y-1.125
N51 G02 X2.375 Y-1.745 I-0.62
N52 G01 X1.625
N53 G02 X1.005 Y-1.125 J0.62
N54 G01 Y-1.02
N55 G03 X0.9363 Y-0.894 I-0.15
N56 G01 X0.9313 Y-0.8909
N57 X0.9271 Y-0.8885
N58 X0.9228 Y-0.8862
N59 X0.9185 Y-0.8841
N60 X0.9141 Y-0.8821
N61 X0.9096 Y-0.8803
N62 X0.9051 Y-0.8786
N63 X0.9006 Y-0.8771
N64 X0.8955 Y-0.8756
N65 X0.8902 Y-0.8742
N66 X0.8855 Y-0.8732
N67 X0.8808 Y-0.8723
N68 X0.8761 Y-0.8715
N69 X0.8714 Y-0.8709
N70 X0.8668 Y-0.8705
N71 X0.862 Y-0.8702
N72 X0.8569 Y-0.87
N73 X0.8541
N74 G03 X0.8163 Y-0.9072 I-0.0003 J-0.0375
N75 G01 X0.816 Y-0.9447
N76 Y-0.9492 Z-0.0597
N77 Y-0.9537 Z-0.0589
N78 X0.8159 Y-0.958 Z-0.0576
N79 Y-0.9621 Z-0.0557
N80 Y-0.966 Z-0.0534
N81 Y-0.9696 Z-0.0506
N82 X0.8158 Y-0.9728 Z-0.0474
N83 Y-0.9756 Z-0.0438
N84 Y-0.9779 Z-0.0399
N85 Y-0.9798 Z-0.0358
N86 Y-0.9811 Z-0.0315
N87 Y-0.9819 Z-0.027
N88 Y-0.9822 Z-0.0225
N89 G00 Z0.2
N90 X0.525 Y-0.1425
N91 Z0.14
N92 G01 Z-0.0206 F13.333
N93 Z-0.0225
N94 G19 G02 Y-0.18 Z-0.06 J-0.0375
N95 G01 Y-0.2175 F40
N96 G17 G03 X0.5625 Y-0.255 I0.0375
N97 G01 X1.45
N98 G02 X1.5349 Y-0.2901 J-0.12
N99 G01 X1.6599 Y-0.4151
N100 G02 X1.695 Y-0.5 I-0.0849 J-0.0849
N101 G01 Y-0.87
N102 G03 X2.305 I0.305
N103 G01 Y-0.5
N104 G02 X2.3401 Y-0.4151 I0.12
N105 G01 X2.4651 Y-0.2901
N106 G02 X2.55 Y-0.255 I0.0849 J-0.0849
N107 G01 X3.
N108 X3.4375
N109 G03 X3.475 Y-0.2175 J0.0375
N110 G01 Y-0.18
N111 G19 G03 Y-0.1425 Z-0.0225 K0.0375
N112 G00 Z0.6

N113 M05
N114 M09
N115 G30 P02
N117 M02
%

[Anonymous]

Im onto something...  I ran my probe to the tool setter...  Z was out .020"

How the hell does that happen lol???  I've never smashed the thing...  I guess I should see if the stylus is loose??

[lenny_1962]

(T996 D=0.375 CR=0. TAPER=45deg - ZMIN=-0.06 - chamfer mill)
N1 G40 G80 G90 G94 G17
N2 G20
N3 G30 P02

(2D Contour9)
N5 M09
N6 G116 T996
N7 S5000 M03
N8 G15 H30
N9 M08
N11 G00 X3.1861 Y-0.9819
N12 G56 Z0.6 H996
N13 Z0.14
N14 G01 Z-0.0206 F13.333
N15 Z-0.0225
N16 Y-0.9816 Z-0.027
N17 Y-0.9808 Z-0.0315
N18 Y-0.9795 Z-0.0358
N19 X3.186 Y-0.9776 Z-0.0399
N20 Y-0.9753 Z-0.0438
N21 Y-0.9725 Z-0.0474
N22 X3.1859 Y-0.9693 Z-0.0506
N23 X3.1858 Y-0.9657 Z-0.0534
N24 Y-0.9618 Z-0.0557
N25 X3.1857 Y-0.9577 Z-0.0576
N26 Y-0.9534 Z-0.0589
N27 X3.1856 Y-0.9489 Z-0.0597
N28 X3.1855 Y-0.9444 Z-0.06
N29 X3.1849 Y-0.9069 F40
N30 G03 X3.1469 Y-0.87 I-0.0375 J-0.0006
N31 G01 X3.1403 Y-0.8701

yours says the Z for the chamfer mill goes down to Z-.06.

when you run the cutter without a part in what does it say in the control?

if it say -,06 sounds like your cutter isn't zero'd correctly...???

[Anonymous · Accepted solution]

I ran the probe to the toolsetter... it was out .020"..  That was the problem.

I have no idea how or why however.  The probe has not been crashed or mishandled.  I need to look into this a bit more.

[al.whatmough]

Thanks for circling back on this for us!

Keep us posted if that is not the issue.

[Greg_Haisley]

@Anonymous  The next time you run a new program for the first time try this tip to avoid scraping any parts.

  We always increment the tool up in Z with the tool length offset at the control by .05 or so. You can post only the chamfer tool by itself so you won't have to restart the program in the middle, which can be a hassle if the restart info is incorrect. Keep recutting the part and modifying the tool length offset until you get the chamfer you want. Then you can go back to the CAM and adjust the tool tip width or the stock to leave setting to get a correct part the first time. This is standard practice in my shop. A whole lot cheaper than scraping parts.

In theory this procedure will work for machining centers or turning centers. It's a practice I was taught by one of the smartest CNC programmers I know back in 1980.

Good luck,

Greg Haisley

Camtool Inc.

[lenny_1962]

Greg did he also teach you how to read tape .........;-P

[Greg_Haisley]

Good one Lenny!

He would not let us make any edits unless he approved. He programmed lathes and mills using a Tandy Radio Shack trs80 computer with a black and white monitor and floppy drives with a ABCD RS232 manual switch box. This was 3 years before IBM came out with the PC. 

[al.whatmough]

@Greg_Haisley   

Greg,

This is a great tip.  Chamfer tools can be the hardest to pick up and just the difference of a few thou makes can make a great part look like crap!

[Greg_Haisley]

@al.whatmough  Thanks - works great for those pesky corner rounders also - where to get it right the user may have to adjust both the length and diameter offsets to get the perfect part.

[lenny_1962]

---

@Camtool-Ind wrote:

@al.whatmough  Thanks - works great for those pesky corner rounders also - where to get it right the user may have to adjust both the length and diameter offsets to get the perfect part.

---

@Greg_Haisley

guys forget that is how you set them on a manual mill, just do it the same for CNC.

i knew that after getting his SW files and seeing that the toolpath and post were correct that the OP had a setup problem, hopefully he'll check his setup sooner next time from this experience.

[Anonymous]

All this new (new to me) technology... I'd have never thought that the probe was out...hell it's only 3 weeks old... Lol.

Thanks for all the tips!

[Laurens-3DTechDraw]

@Anonymous

One thing I can guarantee you is that everything will walk in a machine.

Probe's, offsets, everything moves over time. That's why I measure my tool probe at least once a month.

After that check the length of work offset probe. And then recalibrate the 4 and 5 axis.